Smitty, are you going to write your programs by hand? Are you good with a calculator, and do you understand a bit of trigonometric functions?
I'd highly recommend you get some software to help you out, maybe Bobcad 17 would do for a start, yet be quite cheap.
I haven't gathered from the discussions exactly what TurboCNC expects for arc parameters but here is the general rule: from wherever your machine (tool) is positioned right now, an arc command needs to contain an X and a Z coordinate for the endpoint of the arc coming up, plus it needs an I and a K coordinate to tell it where the center of the arc's radius is located.
If your machine can move a maximum of 90 degrees per arc command, then it needs no G02 or G03 to tell it the direction to move around the circle, this is typical of some controllers. However, usually a G02 or a G03 is needed to command the direction clockwise or counterclockwise movement when the arc is being traversed.
So
G02 Xx.xxx Zz.zzz I.iii Kk.kkk
is what the generic command would look like. I corresponds to the X coordinate of the arc center, and K corresponds to the Z coordinate of the arc center.
Some controllers will instead accept a R parameter which is the radius, so you would see
G03 Xx.xxx Zz.zzz Rr.rrr
Some controllers are very exacting about the accuracy of the arc center coordinates, and high precision is required for the calculation. The controller checks it current position, looks at the end coordinate of the arc, and then determines whether it can actually get there if the center is where you have specified. If not, then it may give you an error, and not move at all, or else, it will make a correction (linear movement) at the end of whatever portion of the arc it does attempt to do, which will create a gouge or something undesirable in your toolpath.
When you make the calculations for the arc coordinates, you need to know whether the controller expects the arc center coordinates to be in absolute coordinates (from a main part zero point), or incremental coordinates (point to point movement).
In addition, for lathe tools, you need to make a tiny allowance for the tool nose radius of the insert you are cutting with. Since your toolpath is typically planned for a theoretically sharp point, this means in real life, that if you use the "sharp point path" for a final path, the radii you cut will be slightly larger than the specification, let's say by .015 to .031 inch, as these are typical tool radii.
So then, you need to allow for this by drawing your part paths slightly undersize by the amount of the tool nose radius. Or, use tool nose radius compensation at the controller to do this for you on the standard full-scale part profile.
One other trick in lathe programming is of course, that X is usually a diametral figure (Z is not) rather than the actual length of the radius, so a quarter circle starting on the centerline at X0Z0 and moving through a 90 degree sweep on a 1" radius, would be written something like
G02 X2.000 Z-1.000 I0.000 K-1.000. If X were a radius value then you wouldn't have to remember to double the X values all the time.
Now you know why you need some software to give you a hand
